structural design of an instrumented double-swept wind tunnel model

12 Pages·2015·20.02 MB·English

20th International Conference on Composite Materials
Copenhagen, 19-24th July 2015
STRUCTURAL DESIGN OF AN INSTRUMENTED DOUBLE-SWEPT
WIND TUNNEL MODEL

Benjamin Lütke1*, Moritz Schmidt2, Julian Sinske1 and Jens Neumann1

1Institute of Aeroelasticity, German Aerospace Center (DLR)
Bunsenstraße 10, 37073 Göttingen, Germany
*Email: [email protected], web page: http://www.dlr.de

2Engineering Facility Systemhaus Technik, German Aerospace Center (DLR)
Lilienthalplatz 7, 38108 Brunswick, Germany

Keywords: Wind Tunnel Model, Finite Elements, Modal Analysis, Fluid-Structure Interaction
Simulation, Strength Analysis, Helicopter Rotor Blade Tip

ABSTRACT
The design of a highly instrumented, double-swept CFRP wind tunnel model and its experimental
setup are presented. A forced sinusoidal pitching motion is applied to the one-sided clamped helicopter
rotor blade tip. Challenges of the structural design and the manufacturing process are addressed. A
mold with inserts to check the leak-tightness of the pressure transducers and retain the half shells in
the mold is presented. Insights in the finite element analysis (FEA) of the blade tip model are given.
The strength analysis reveals peak stresses in the adhesive and the spar. The finite element model is
validated with an experimental modal analysis. The experimental and numerical mode shapes and
eigenfrequencies show an excellent agreement. The design goal of a very stiff lightweight model is
met with the first eigenfrequency at 70 Hz. The results of the fluid-structure interaction simulation at
Ma=0.4 show no significant differences for the global forces compared to the simulations with the
rigid contour. However, the maximum tip deformation is up to 20 mm and a slight excitation of the
first bending mode can be observed.

Figure 1: Model with optical markers in wind tunnel test section (left); View of installation (right)

1 INTRODUCTION
In fast forward or maneuvering flight, dynamic stall at the retreating blade of a helicopter leads to
high pitching moments and can even limit the flight envelope. The dynamic stall behavior is difficult
to predict and has been fully understood only for a few advanced blade tip planforms like the BERP
[1]. Double swept helicopter blade tips have shown the potential to reduce noise and vibrations [2].
However, the understanding of the three-dimensional dynamic stall behavior is still limited. A new
B. Lütke, M. Schmidt, J. Sinske and J. Neumann
aeroacoustically improved planform of AIRBUS-helicopters [3] is chosen for the experimental
investigation in the Transonic Wind Tunnel Göttingen. In the non-rotating experiment, a forced
pitching motion simulates the angle of attack variation of the once-per revolution motion of the
helicopter rotor blade. This allows the influence of aerodynamic parameters on the complex flow to be
investigated with high accuracy. Subsequently, computational fluid dynamic simulations (CFD) and
fluid-structure interaction simulations can be validated. Comparisons to rotating cases can be made by
means of simulations in a second step.
One design goal for the experimental investigation is a very stiff lightweight model in order to
reduce its aeroelastic influence on the flow and limit the inertial loads. Due to a high aspect ratio with
small cross sections and a high degree of instrumentation a carbon fiber reinforced plastic (CFRP)
model is chosen as the best solution. Many CFRP models with more complex configurations have
been presented in the past, e.g. active flaps [4]. The originality of this paper derives from the detailed
insights in the structural design and the manufacturing process including instrumentation issues. The
strength analysis with the high fidelity finite element model reveals the highest stress exposures in the
spar due to the ribless construction. Although, the presented numerical and experimental modal
analyses are standard, the importance of using the original clamp condition is striking. Correct
numerical mode shapes and eigenfrequencies are essential for the fluid-structure interaction (FSI)
simulations that are based on a modal approach. The presented FSI simulation at a pitching frequency
of f=6.6 Hz is compared to a CFD simulation with a rigid contour.
In the first part of the paper, the experimental setup is described. In section 3, the geometry and the
expected aerodynamic loads of the rotor blade tip are shown. Detailed insights into the structure and
the manufacturing process are given in section 4. The finite element analysis including the numerical
and experimental modal analysis is presented in section 5. Finally, a first unsteady fluid-structure
interaction simulation is shown.

2 EXPERIMENTAL SETUP
The Transonic Wind Tunnel Göttingen (DNW-TWG) has a closed test section with a cross section
of 1m x 1m, see Figure 1. The lower and upper wall can be adapted. Mach Numbers from (cid:1839)(cid:1853)=0.3-0.9
are feasible. Total pressures from (cid:1868) =0.3-1.5 bar can be adjusted. A maximum temperature of
(cid:2868)
(cid:1846) =323 K is expected at the model. The forced pitching motion is applied by a hydraulic test
(cid:2868)
oscillation rig outside of the test section. The possible oscillation amplitude decreases for increasing
pitching frequency. For sinusoidal motion the limit of the amplitude is (cid:2009) (cid:3404) 4° for the maximum
(cid:3040)(cid:3028)(cid:3051)
target frequency (cid:1858) =13.2 Hz whereas for the target frequency (cid:1858)=6.6 Hz the limiting amplitude is
(cid:3040)(cid:3028)(cid:3051)
(cid:2009) (cid:3404) 8°. A piezo balance with four three-component piezo elements is mounted between the
(cid:3040)(cid:3028)(cid:3051)
oscillation rig and the model in order to measure the global forces and moments. The angle of attack is
measured by means of two laser triangulators pointing on a cantilever beam of an aluminum disc
mounted between the model flange and the piezo balance (Figure 1). A gap of 1.5 mm between the
cylindrical part of the model flange and the wind tunnel wall inserts ensures contactless operation.
Aerodynamic covering plates of 0.4 mm thickness are bonded on the model flange on the inside of the
wind tunnel in order to limit side flows from the plenum chamber.
Sixty unsteady pressure transducers are installed in the model to get discrete pressure data of high
accuracy. The distribution of sensors is shown in Figure 2 on the left. The motion of the model is
monitored by two accelerometers inside the model and by an optical marker measurement system.
Two temperature sensors inside the model are used for the calibration of pressure sensitive paint, an
optical measurement method which is used to receive surface pressure information in the experiment.
The sensor systems described above have to be considered in the design phase with regard to space for
instrumentation and cable feedthrough.

3 GEOMETRY OF THE WIND TUNNEL MODEL AND EXPECTED AERODYNAMIC
LOADS
A maximum span s=750 mm is chosen in order to limit the aerodynamic interference of wind
tunnel wall and tip vortex. The planform, shown in Figure 2, is adapted from a parametrized AIRBUS-
HELICOPTER patent [3].
20th International Conference on Composite Materials
Copenhagen, 19-24th July 2015

Figure 2: Planform, twist and sensor distribution from [5] (left); Aerodynamic load case (right)

A high aspect ratio of AR=4.5 is required to resolve flow separation at high angles of attack
inboard of notch. The forward sweep of Λ (cid:3406)11° begins at r=200 mm and ends at r=390 mm. The
chord length (c=165 mm) is nearly constant until the latter position. With the beginning of the
backward sweep of Λ (cid:3406) 25.7° the chord length linearly decreases to c=106 mm at r=638 mm. The
parabolic tip shape leads to a minimal chord length of c =47.5 mm at the tip. The model has no
min
anhedral in order to reduce optical measurement complexity. The twist distribution of a realistic
helicopter rotor blade usually decreases from the root to the tip due to the varying inflow velocity
along the blade. The twist distribution of the wind tunnel model, as shown in Figure 2, is decreased at
the root so that the first separation inboard of the notch is not triggered by the wind tunnel wall
separation.
The airfoil EDI-M112 with 12% thickness is used for the inner unswept part while the airfoil EDI-
M109 with 9% thickness is used for the forward/backward swept part [5]. Consequently, the maximal
thickness of the blade is 16 mm. The trailing edge of the outer part is thickened to allow a minimum
thickness of t =0.5 mm.
min
A typical unsteady aerodynamic load case at (cid:1839)(cid:1853)=0.4 and (cid:1844)(cid:1857)=1200000 is shown in Figure 2 on the
right. The unsteady CFD-simulation with rigid contour leads to a maximum lift force of F =1313 N
Z
whereas the steady lift peak remains at F =1180 N. Therefore, the maximum loads of the unsteady
Z
simulation are used for the strength analysis presented in Section 5.3. Besides the calculation of the
global loads, the aerodynamic flow phenomena are investigated by means of the CFD-simulation, see
[6].

4 STRUCTURAL COMPONENTS AND MANUFACTURING OF THE CFRP-MODEL
Several requirements lead to a carbon fiber reinforced plastic design of the wind tunnel model:
 The high bending and torsional stiffness needed to limit the aeroelastic influence on the flow
 A lightweight construction for low inertial loads due to the forced motion
 The high aspect ratio which leads to a small chord length and reduces the space for
instrumentation and cable feedthrough.
The two CFRP half shells with integrated spar caps, shown in Figure 3 on the right, carry the main
bending loads. One central spar resists shear forces and prevents buckling. Torsional loads are carried
by the closed shell and the central spar. A hollow steel shaft is adhesively connected to the shells and
the spar at the model root and transfers the loads to the hydraulic oscillation rig (Figure 1). Vacuum
bag molding is used for all composite parts of the model.
B. Lütke, M. Schmidt, J. Sinske and J. Neumann

Figure 3: Aluminium mold with removable inserts (left, mid); Full instrumented half shells (right)

The upper and lower half shell are hand layed in the aluminum molds shown in Figure 3 on the left.
The high surface quality with (cid:1844) (cid:3407) 3 μm along with the robustness and the reusability compensate the
(cid:3053)
high costs of the mold. Each mold has five hollow, removable inserts which are distributed along the
wingspan including the main instrumented sections. Thus, the holes for the discrete pressure
measurements with a diameter ∅ (cid:3404) 0.3 mm can be drilled from the half shell through the inserts. Due
to the cavity of the inserts, the pressure transducers are not destroyed by overpressure when inserting
them into the brackets (Figure 4). Furthermore, the leak-tightness can be tested during the
manufacturing process. In case of an unwanted detachment of the half shells the inserts can be
removed from the mold while the half shells are retained in the mold by partial vacuum for the final
bonding process.

Figure 4: Detail of instrumentation at the notch (left); Sketch of spar cross section (right)

The high modulus, unidirectional M46J-lamina and the epoxy LR385 are used for the half shells. In
order to avoid dry spots, a maximum fiber volume fraction of 50% is chosen for the complex
geometry. The symmetric ply layout is listed in Table 1. Ply 7-18 are the integrated spar caps which
are orientated 2.5° in forward direction in order to follow the spar contour and enforce the bending-
torsion coupling. The spar caps have a chordwise tapering of 8:1 and taper out right behind the notch.
The approximate position of the spar caps is shown in Figure 10 on the left. A spanwise tapering of
26:1 is used at the steel shaft to reduce stress concentrations and transfer loads smoothly from the half
shells to the steel shaft. Plies 3-4 and 21-22 are dropped at the beginning of the parabolic tip since
loads decrease in tip direction and instrumentation space is limited due to the tapered geometry. The
first and the last six plies as well as the integrated spar caps are laminated in separate steps. The fiber
volume fraction is met precisely to ensure strength and the correct thickness for perfect integration of
spar and steel shaft. An adhesive gap of 0.4 mm between the components is not exceeded. The holes
20th International Conference on Composite Materials
Copenhagen, 19-24th July 2015
for the pressure transducers and the corresponding brackets are drilled before the other parts are glued
to the half shells.

Table 1: Layup of upper and lower half shell at position of integrated spar caps – HM lamina M46J

Layer 1 2 3 4 5 6 7-18 19 20 21 22 23 24
Orientation
-45 45 90 0 23 -23 -2.5 -23 23 0 90 45 -45
in °

The contour of the central spar follows the contour of the blade tip. The milled foam core
(ROHACELL) is covered with two C-shapes (cid:3399)45° weave Style469, see Figure 4. The C-shapes of the
weave end right before the heightening of the foam core which indicates the thickness limit of the spar
for optimal integration into the half shells. An exact fiber volume fracture of =50% is difficult to meet
since the weave is not easy to be fixed on the core with its small dimensions and radii.
Only one pressure transducer is placed at the position of the spar to not weaken the weave. A notch is
cut in the foam core and the weave is laminated along this notch. The spar has an upper and lower
overlap to the steel shaft for a more homogeneous stress distribution. The upper overlap is laminated
on the spar by means of a plastic support construction. After the spar with the upper overlap is bonded
to the upper shell, the steel shaft is glued in place. Then, the lower overlap is laminated on the spar and
the steel shaft. Before the pressure transducer brackets are glued in the half shells with epoxy, the
leading edge (LE) support structure is glued in the upper shell. Cut outs at the positions of the
transducers and the brackets are provided. The pressure transducers are glued in the brackets with
silicone due to its vibration resistance. Silicone is also used to fix the cables and transducers in the half
shells (Figure 4).
For the LE support structure, a support shell is laminated in the front part of one original aluminum
mold. A carbon half mold is laminated on the outer contour of this support shell and connected to the
other original aluminum mold. Finally, the LE support structure is laminated to the U-contour of the
original aluminum mold and the connected carbon front mold. The original specified weave “Style 452
- T 700 SC” could not be used neither for the weave of the spar nor for the LE support structure
because it turned out to be too stiff to fit on the small radii during laminating.
The steel shaft is milled of a 42CrMo4 steel block. It has one main channel for cable feedthrough
and one spanwise and chordwise channel in order to reduce stress concentrations and save weight.
Milled slots are provided for the spar overlap. The steel shaft is fixed with 4 M10 screws to a distance
disk with cantilever beams where the angle of attack is measured with two laser triangulators, see
Figure 1. Two hole patterns are provided for different angles of incidence. The distance disk is fixed
with 16xM6 screws to the Piezo balance on the hydraulic test oscillation rig so that the forces are
homogeneously distributed to the 4 Piezo elements. An external centering is provided between the
steel shaft and the disc, an internal centering between balance and disk.

Figure 5: Spanwise measured deviation: upper surface 15 mm in front of the TE, resolution: 10 mm

After the final bonding procedure, the model is cured for 15 hours at 55°C. The surface contour
shows a slight thickening of about 0.1 mm compared to the reference contour. One measured spanwise
cross section of the upper surface is shown in Figure 5. However, no signs of the inserts of the mold
can be seen.
B. Lütke, M. Schmidt, J. Sinske and J. Neumann
5 FINITE ELEMENT ANALYSIS AND VERIFICATION
A high-fidelity finite element model based on a linear approach is established in ANSYS-APDL.
The unsteady CFD-load case at (cid:1839)(cid:1853)=0.4 and (cid:1844)(cid:1857)=1200000, see Figure 2, is used for the strength
analysis presented hereafter. The experimental modal analysis is compared with the numerical results
to verify the finite element model and to define possible adaptions to the finite element model.

5.1 FE Modeling
Four different element types are used for the finite element model: the 8-node layered shell element
SHELL281, the 20-node solid element SOLID186, the 2-node beam element BEAM188 and the rigid
region link CERIG [7].
In Figure 6 the modeling is shown in detail: the laminate of the half shells, the leading edge support
structure and the weave cover of the spar are modeled with layered shell elements. The steel shaft, the
foam core of the spar and the adhesive are modeled with solid elements.

Figure 6: Finite element modelling of the wind tunnel model (distorted illustration of the airfoils)
20th International Conference on Composite Materials
Copenhagen, 19-24th July 2015
Different modeling approaches for the adhesive and the connection between solid and shell
elements have been presented in [6]. In the final modeling approach presented in this paper, the
structured shell elements simulating the upper and lower half shell are placed on the outer contour.
The (cid:1872)=0.3 mm thick adhesive between the steel shaft and the half shells is modeled with solid
elements. The elements are placed on the faces of the unstructured solid elements of the steel shaft.
The free faces of the adhesive on the opposite site of the half shells are structured and have the same
node distribution as the structured elements on the half shells. The nodes are linked by CERIG-
elements with the length of the final laminate thickness.
The structured shell elements simulating the weave of the spar are placed on the faces of the
structured solid elements simulating the foam core. The opposite nodes of the solid elements
representing the adhesive are linked to the nodes of the spar via a distance equal to the weave
thickness (cid:1872)=0.7 mm by CERIG elements. The nodes on the other side of the (cid:1872)=0.4 mm thick adhesive
are linked to the nodes of the half shell elements by CERIG elements.
The leading edge support structure is modeled with shell elements which are connected to the shell
elements of the half shells by solid elements, with the property of the adhesive. This leads to an
overrated bonding thickness which reduces stress peaks in the adhesive.

Figure 7: FE - modeling of boundary conditions wind tunnel boundary condition

The wind tunnel clamp is modeled with beam elements which have the material properties of steel, see
Figure 7. At the position of the bearings the nodes are fixed: one is simulated as a fixed bearing with
all degrees of freedom fixed, the other is simulated as a floating bearing with fixed displacements in x-
and z-direction. The cross section of the beam elements reflects the cross section of the driving axis.
However, the disc with the cantilever beam (Figure 1) is not included in the FE model. Furthermore,
the rigid links between the last beam element and the solid elements of the steel shaft might lead to a
too stiff behavior of the numerical model. Thus, the modeling shown in Figure 7 is rather a rough
approximation of the real boundary condition.

5.2 Numerical and experimental modal analysis
The numerical and experimental modal analyses are performed with two different boundary
conditions. The first is the clamped condition in the wind tunnel, shown in Figure 1 and Figure 7. The
experimental part of this modal analysis is done hours before the wind tunnel experiment starts, so
these data cannot be used for a finite element model validation which supports the strength analysis
required for the wind tunnel test. The second is the model clamped to a solid steel block, as shown in
Figure 8. In this setup the model is easily excited with either a shaker or with an impact hammer. This
experimental modal analysis is used for the finite element model validation a long time before the
wind tunnel experiment.
B. Lütke, M. Schmidt, J. Sinske and J. Neumann

Figure 8: Experimental modal analysis on a solid steel block and FE modeling of boundary condition

The experimental results, presented in Table 2 and Figure 9, are produced by means of the impact
hammer. The clamped support of the wind tunnel on the one hand and the steel block on the other
hand explain the differences between the eigenfrequencies corresponding to the two boundary
conditions. The stiffer clamped support of the steel block leads to higher eigenfrequencies in general.
The realistic FE-modelling of the boundary conditions shown in Figure 8 leads to good agreements
between the numerical and experimental results in case of the steel block. The modal assurance
criterion (MAC) is greater than 93% for the first four mode shapes and even the 6th mode shape has a
MAC-value of 78%. For the comparison of the numerical and experimental mode shapes the
correlation coefficient presented in [8] is used. The results might be further improved by integrating
the masses of sensors and cables. The discrepancies between the numerical and experimental results in
case of the wind tunnel clamp are due to the imprecisely simulated model connection. However, these
modes reflect the experimental wind tunnel clamp condition better than the fixed boundary condition
in case of the steel block, shown in Figure 8. Therefore, they are used for the first fluid-structure
coupled interaction simulation.

Table 2: Experimental and numerical eigenfrequencies for different boundary conditions

Mode Number 1 2 3 4 5 6
Numerical Frequency in Hz 69.4 198 299 429 499 752
Clamp Steel
Block
Experimental Frequency in Hz 69.6 196 275 434 463 729
Numerical Frequency in Hz 67.7 181 201 369 430 530
Clamp Wind
Tunnel
Experimental Frequency in Hz 67.3 153 186 273 466 515
20th International Conference on Composite Materials
Copenhagen, 19-24th July 2015

Figure 9: Experimental (blue arrows) and numerical (surface solution) results of the modal analysis

5.3 Strength Analysis
For the strength analysis, unsteady CFD-simulations with a rigid contour are carried out. The load
cases with the estimated highest loads are simulated and chosen for the strength analysis. The loads at
the point of the highest lift are extracted and applied statically on the finite element model. The
solution is superposed on the harmonic analysis. In the harmonic analysis the harmonic motion is
applied on the model only. The procedure and details of the CFD-simulations are described in [6]. The
loads are interpolated from the CFD grid to the FEM grid by means of radial basis functions. The load
case used for the strength analysis presented in the following is shown in Figure 2. The model is
exposed to a forced pitching motion ((cid:1858)=6.6 Hz, (cid:2009)=10(cid:3399)8°) at (cid:1839)(cid:1853)=0.4 and (cid:1844)(cid:1857)=1200000. The loads
are extracted at the instantaneous angle of attack (cid:2009) =16.47°.
(cid:3036)(cid:3041)(cid:3046)(cid:3047)

Figure 10: Stress exposure: FF - upper shell (left); IFF – lower shell (right)
B. Lütke, M. Schmidt, J. Sinske and J. Neumann
For the strength analysis of the half shells the Puck criterion [9] is used. It identifies fiber failure
(FF) and inter-fiber failure (IFF) in the unidirectional M46J lamina listed in Table 1. The out-of plane
properties of the M46J lamina and the four Puck inclination parameters are estimated with data from
similar materials while the other material properties are determined experimentally. The upper half
shell is more critical to fiber failure then the lower half shell since the compressive strength in fiber
direction is approximately half as much as the tensile strength. The highest physical relevant stress
peaks occur at the spanwise end of the steel shaft in the 0°-2.5°-layers. The stress exposure of the spar
cap layers is shown in Figure 10. Higher numerical stress exposures can be found in the first +45°
layer due to the modeling discontinuities in the tapering. Therefore, these stress peaks can be
considered lower in reality. Nevertheless, the safety margin has a conservative value of S=2.6. The
lower half shell is most critical to inter-fiber failure in the 90° layers due to negative influence of the
orthogonal tension on inter-fiber failure, as in Figure 10. The safety margin of IFF is S=4.0.

Figure 11: Stress (cid:2026) in shell elements simulating the weave of the LE support structure and the spar
(cid:3052)

The maximum stress criterion is used for the elements simulating the “Style 469 – T 300” weave.
The material properties of the “Style 469 – T 300” weave are adapted from the experimentally
determined properties of the weave “Style 452 - T 700 SC” and other laminates based on the T 300
fiber. The maximum stresses are listed in Table 3. The highest stress exposure or the lowest safety
margin S=2.47 occurs for compressive pressure in fiber direction, shown in Figure 11. The stress is
highest at the position of the notch where most of the pressure transducers are located. Since the
corner radii of the core are not taken into account, the stress peaks are lower in reality. The same holds
for the shear stresses in the bonding on the upper and lower side of the spar, shown in Figure 12.
Therefore, one can assume that the required safety margin S=2 is met assuming a maximum mean
shear stress of (cid:2028) =7 MPa for the adhesive.
(cid:3052)(cid:3053),(cid:3040)(cid:3028)(cid:3051)

Figure 12: Von-Mises stress in steel shaft (left); Shear stress (cid:2028) in bonding, global coordinates (right)
(cid:3052)(cid:3053)